Thank you all for your help. I was hoping I could pick a plane/face and tell it to go in a certain direction and then another face or plane and tell it to go in another direction. I do not want to have to put a cys into the model just to orient. I have all kinds of references already built into the model not including the 3 default planes I already have in there. Also, why would you need to put a cys in when there already is a cys as the default cys.

I understand how to name a view and save. I just cannot get it to where I want it. And no, rotating is not enough.

If you just want to temporarily orient a model a certain way, you can Ctrl+select two perpendicular surfaces or planes and then click the Normal To button on the Standard Views toolbar. The first surface selected will be normal to your screen and the second will be at the top. I use this frequently when I want the model turned a particular way for sketching. The only drawback is that when applying vertical or horizontal sketch relations they will still reference the primary orientation and not how the model is presently oriented.

Thank you all for your help. I am trying to do this "Ctrl pick 2 planes"option. I understand the first pick will be normal to. The second plane will be up. Which side of the plane will be up? I understand if it is a face of the part it will go up but what if all the faces of my part are drafted and none are normal to another because of draft. Then I have to rely on the planes for orientation. Then it becomes important that there are two sides of each plane. Still need help.

Holding ctrl key down and picking 2 planes puts me into a place where I am putting another plane in as another feature. A place I do not want to be. I am dealing with planes ONLY. No part features. I pick one plane to be normal to my screen. This pick alone can put my part either to the right or left depending on where I send my next pick/plane. Which side of the plane on my 2nd pick goes up? You are correct Kelvin. I am over thinking something I should not have to here with SW. I am spending way too much time on something that should be a slam dunk. Unless I am not seeing something here. Pick a side of a plane and tell it to go this way. Pick another side of a plane and tell it to go that way. Thats it. You cannot just say be normal to the screen and then go up with the second pick. That does not work with planes sir. You need planes when you have drafted surfaces and nothing is orthogonal to another.

Still needing help. Perhaps a previous Pro/E user can chime in and help me out with what I am trying to do please.

I understand if it is a face of the part it will go up but what if all the faces of my part are drafted and none are normal to another because of draft. Then I have to rely on the planes for orientation.

Faces do not have to be perpendicular (normal to) each other for the double selection method to work, and the faces don't even have to be adjacent.

Sid Humphreys wrote:

Kelvin,

Holding ctrl key down and picking 2 planes puts me into a place where I am putting another plane in as another feature. A place I do not want to be. I am dealing with planes ONLY. No part features. I pick one plane to be normal to my screen. This pick alone can put my part either to the right or left depending on where I send my next pick/plane. Which side of the plane on my 2nd pick goes up? You are correct Kelvin. I am over thinking something I should not have to here with SW. I am spending way too much time on something that should be a slam dunk. Unless I am not seeing something here. Pick a side of a plane and tell it to go this way. Pick another side of a plane and tell it to go that way. Thats it. You cannot just say be normal to the screen and then go up with the second pick. That does not work with planes sir. You need planes when you have drafted surfaces and nothing is orthogonal to another.

Still needing help. Perhaps a previous Pro/E user can chime in and help me out with what I am trying to do please.

Thanks all.

As Mark pointed out, planes do not work for this method. You have to use faces.

Pick any two of the coloured faces in the attached model to see what happens.

All of the Pro/E users reading this are just as frustrated as you - and all of the SWX gurus reading this arer just as confused as one another.

I want a SWX guru who was / is a Pro/E guru to chime in. I will be one eventually - I have only 18 months on SWX. I completely comiserate with you. Unfortunately I am reading this and all the other posts on this (model orientation, view orientation and sketch orientation) because I, too, am frustrated. This should be simple and included in the software implicitly. SWX programmers decided it was not used enough to implement - if they even thought about it. All the SWX users I know ask "why would you need that?"

Very frustrating...

What's more - I cannot even get the "first pick, ctrl-second pick to work. It ignoes my first pick and puts my 2nd pick parallel to the screen.

A plastic box sit on the table. The lid / box interface is tilted toward the user. The parting line in the mold is tilted with respect to the table surface. The part wants to be modeled sitting on the table, but sketches want to have their vertical orientation normal to the parting plane. So when I sketch a horizontal line, I want it parallel to the parting plane - not the table top. I find that SWX users are just used to the limitation and draw lines "parallel" and "perpendicular" to the parting plane and deal with the skewed reference. This is just extra work from a Pro/E user's standpoint. Because Pro/E let's you tell it which way is up - SWX assumes that direction for you. Pro/E since WF2 (?) assumes a direction as well, but let's you change it via the dialog in my screenshot. Before that it required that input for every sketch.

I hear you... It is NOT a big deal... Just one of those things that is really noticable only after it is taken away.

Like feature numbers in the model tree - SWX users don't see it as a benefit because they're used to floundering around in the tree looking for that feature they need. Pro/E users are accustommed to mentally noting the feature number and can navigate back to that same roound in 2 seconds. Everything in the tree is numbered sequentially so things are easy to find.

Believe me, I have long lists of things that I love / hate about both packages.

First the modify sketch tool (Tools==>Sketch Tools==>Modify...") allows you to flip the side of the plane the sketch is on (although it just looks like you're mirroring the sketch geometry) and rotate the coordinate system to an input value. It's not as good as being able to use a reference but it might give you a way to set up your sketches to your liking.

For this and the feature numbering issue, I encourage you to submit enhancement requests.

I've gotten in the habbit of naming features and organizing them into folders, but even so, I do find myself relying heavily on 'goto feature in tree' in the graphics area when the feature list starts getting long.

John - thanks for the Modify Sketch tip - so THAT''S how you flip the sketch... nice. I needed that yesterday ( I assume it works for Derived Sketches as well...?) Modify Sketch is also an adequate workaround for sketching horz/vert (or sketching text that is upright) at a different angle as long as you can enter the exact angle of rotation. But I really think it is a shortcoming to not be able to tell the software which end it up... For views and sketches alike. I have trouble with it and hopefully will soon get used to how SWX does it.

As for the tree, simply clicking on the feature brings you there in the tree - I really like that (no need to RMB>go to feature). But if two features are separated by more than a screen's length, clicking on one and then the other does not easily tell you which feature is earlier. Any hints on that? - How to tell relative location of features in the history?

No hints on telling which feature comes first in a long tree. You really should submit and enhancment request to have that information report-maybe at the status line)

Modify sketch does work with derived sketches. One caveat, it won't work on sketches with external relations, so if you have a sketch with a line collinear to a plane that you want to flip, you'll need to delete the collinear relation, and then recreate it after flipping the sketch.

Your horizontal orientation issue would also make a good enhancment request. In 2014 they've enhanced plane creation in a way consistent with your description, but I can't talk about that outside of the Beta forums.

Picking on features and having them highlight in the feature manager tree works in part mode pretty well. In an assembly, picking a face on a part highlights the part. That's usually when I'll use the rmb menu item, "Goto feature in tree"

One hint that might help you determine what feature comes further up/down in the tree from another is to look at the position of the scrollbar indicator in the middle of the tree scrollbar. I know it's not as direct as numbering all the features, but it may be helpful if you haven't noticed it before.

Not sure what you meant by "normal to", but I think of "normal" as perpendicular or 90 deg to. When I pick the first face and then the second, the first pick is parallel to my screen and then the second goes to the top of my screen.

Not sure what you meant by "normal to", but I think of "normal" as perpendicular or 90 deg to. When I pick the first face and then the second, the first pick is parallel to my screen and then the second goes to the top of my screen.

Unfortunately, it only works with faces, not planes so I can't think of a way to do exactly what you want except for:

Use a face that gets you the correct normal view and a second face that gets you to some angle that is an increment of the Alt-arrow key rotation angle away from the desired top up orientation and then use the alt-arrow keys to get it into the desired rotation. See the blog post I referenced for alt-arrow key usage.

Create some "construction" surface or solid geometry to make faces that you can use to orient the model. Surfaces are probably better since they won't affect mass properties, you don't have to worry about merging to your regular model, etc. and you can just hide them after using them.You can also use solids if desired (with the merge option turned off) and then use the delete body command to have them not affect the mass properties, but still keep them in the model history for reference.

Jim I appreciate you trying to help me. I think you see what I am trying to accomplish though. I did read the arrow key orientation piece too.

I really think SW needs to add the capability to orient by planes. Like I said, when you have plastic drafted part surfaces or faces, these are not the best way to go. And if I have to go and create additional geometry no matter how easy SW says that is, just to orient a part, that becomes a hassle. Even if I only have to do it once. I do not want to have to count or hope for correct increments of arrow keys.

No apologies necessary Glenn. We are all doing the 9 to 5 grind and just trying to do our job with the "hammers" we are supplied with. I am eternally grateful for every bit of help you all have given me. And I do mean that. I needed SW basic training weeks ago from my new company and they tell me it is coming. But up until then you guys are all I have. I am coming from a 20 something year background of all Pro/E and things are just a tad different here. I do not mean to come off as stubborn at all and I apologize if it seems as if I do. Just trying to get the job done under time constraints as we all are.

Again guys, thank you very much for putting up with my questions and history. I'll see if I can get a stipend from the company here divvied up for all of your guys to share for all of your help these past few weeks.

The article you linked to was extremely helpful for my specific problem.

I discovered upon trying to make a sheet drawing from my assembly that the assembly itself is sitting at an odd angle (around 20-30 degrees) in relation to the origin/planes. So all of my 2D drawing view options in the view pallete are at the odd angle. So by using this double-select Normal-To feature, I can get the custom drawing views that I am looking for. However it requires me to normal to every side I want to make a drawing view of.

Knowing now that my assembly is lying at an angle, how can I reorient everything in the assembly to the way that I want so that it will be saved in the correct position from here on out? If you hover over the Front Plane, you can see that it is not centered within the plane as it should be (pictured).

Is there an easy fix? The assembly I am using was created in other software, by someone else, and so I am having to make it work for my requirements (fixing broken relations/missing parts). Having reopened the original assembly, I can see that somewhere along the way I must have applied a relation that caused the assembly to shift out of a 90 degree alignment to my screen, because the original assembly is perfect in that respect.

I had view origins turned on, in hopes it would help me reorient a straight line 90 degrees upward, which is all I want. I am unsure why there are so many other origins cluttering the screen though, as I am new to the software.

If the original assembly is oriented nicely and your repaired assembly is out of whack, it should be fairly easy to get it back in line. Is one of the parts fixed (it will have (f) after the icon and before the part name in the feature tree)? If so, you can probably Float that part and then reorient it so that the assembly lines up correctly.